[BlueFin]

I have a need to machine some deep pockets, 6061-T6, pocket is 1.7" wide, 13" long and will be 2.7" deep. I have ordered two new Niagara A337 3 flute 37 degree helix bright finish HSS cutters, one is 1.250" cutting length and the other is 3" cutting length, both are 1/2" diameter. Was going to use a 3/4" drill to remove as much of the pocket as I can first, then manual end mill even more away for a near net size of the pocket and then CNC the finished product. So I think the cutter will only remove about .125" or less from the wall when CNC.

Any suggestions for the feed/speed on the long end mill? right now I am thinking 4500 RPM, 10" IPM and .050" depth of cut. This will take 2 hours with those settings. And that is with the short end mill running at 20" IPM to cut down to 1.125" inches first, then take over at that depth with the long end mill to finish it out.

[SCzEngrgGroup]

Reduce your RPM, and increase your feedrate - Your SFPM is a bit high for HSS (589 FPM), and your chipload is WAY too low (about 0.0007"/tooth). You'll dull your cutter very quickly like that. I would drop the RPM to around 3500, and increase feedrate to around 35 IPM or even higher (you should be able to go up to 60-70 IPM if your machine is rigid enough). Adjust depth and width of cut as required (increasing feedrate with reduced WOC to account for chip thinning) to get a good quality cut. Leave 0.005-0.010" for the final, full-depth pass at slightly higher RPM, and lower feedrate. At full depth, you'll have to take VERY light cuts, to avoid tool flexing. Even then, if your machine isn't VERY tight, and VERY rigid, you likely won't get a great finish.

If the chips aren't coming off HOT, you're feeding too slow, and the tool will heat up and dull quickly.

Regards,
Ray L.

[keen]

Hi Bluefin - I dont see your rad spec - how big a cutter can you use? If you can use an insert cutter with clearance above the cutting zone - see pic - (you can make one to suit alum geometry tips) - and just step it down - I would not rough drill first, just a series of smooth level cuts stepping down.

[BlueFin]

Thanks guys, wow that is pretty good surface finish in that photo. The radius is .130 so a 1/2" end mill can just do the job, the comment about reduction in RPM got me thinking if the slower RPM will reduce chatter? I am just assuming that the long end mill will be all over the place with any kind of heavy cutting at all. Never tried one like that before so this is all new to me.

[zephyr9900]

The radius is .130 so a 1/2" end mill can just do the job,

Please post the gcode for that when you're done, BlueFin. I'm always up for learning a new technique.

the final, full-depth pass

Whenever I try even a thou-or-two finshing cut (even squaring up the end of a work blank, much less pocketing) I always get a "singing" kind of ripply finish when I try a DOC much deeper than about 2 cutter diameters on a 1/2 endmill, even in 6061 or Mic-6.

Even then, if your machine isn't VERY tight, and VERY rigid,

Does that mean a really new, fresh Tormach, or are you talking machines in general?

Randy

[twocik]

I've tested making a full 1.25" pocket with a 1/2" rougher & finishing 1/2" EM. I left .02" for my final wall pass and noticed if I reduce the RPMs I saw a 50% better looking finish. Another thing I noticed was the cutters life was reduce by 10% - 20%.

[tikka308]

what were your S&F and DOC with the 1/2" end mills?

[BlueFin]

I guess I should be awake when I post things here, the radius of the corners is .275" for a .550" diameter. The other radius came from an un-related drawing somewhere My thought with a long end mill is not so much with machine rigidity, but the simple fact that this 1/2" end mill is 3" long! It just seems like it's going to wobble all over the place. And I have heard the ringing effect mentioned with 2" end mills. The idea of lower RPM does seem to make sense, but I only have one shot at this to get it right, the block of aluminum cost $35.00

[BlueFin]

So I just talked with a commercial machine shop owner and showed him the drawing and the end mill, he said that he would run it at 800 RPM and 5 inches per minute, with a .020" finishing allowence, this would be a .002" chip load. He said the longer the end mill the slower you go. Otherwise it will ring like a bell and bother the next door neighbors.

[twocik]

"what were your S&F and DOC with the 1/2" end mills?"

Sorry can't remember that far back, it was just me typing in the MDI playing around, but maybe I'll try it again tomorrow and report back.



"the block of aluminum cost $35.00 "


Bluefin just hit the undo button if it's not to your liken, I use it all the time.


What I've learned was to cut everything in half for longer end mills. However 3" is pretty long, 800 rpms at 5 IPM climb cut sounds about right to me. Not sure how great this would work, but you could try 2 passes at .001" 687 rpms at 1.4 IPM.